## Fluids

#### Fluid flow at high pressure

• pcsingh
Subscriber

Hello all!!

There is a fluid flow problem, the boundary conditions at the inlet are as follows: V= .1 m/sec, T=305 K, Pressure=1300000 pa. I am using the velocity inlet option. What value should I put in the Supersonic /initial Gauge Pressure tab?
The default operating pressure is 101325 pa.

• Rob
Ansys Employee

Is the system compressible?  Read what the Help system tells you: unless you've got supersonic flow at 0.1m/s it's not going to do anything.

• pcsingh
Subscriber

Thank you Rob sir for the reply.

No, the system is incompressible. I am studying a fluid(Refrigerant) out from the condenser of an AC system, where the pressure is at 1320000 pa. This fluid (outlet from the condenser) is the inlet condition for my study. I am also assuming that there is no pressure loss during the study. Here, the fluid is not flowing at normal atmospheric pressure, it is flowing at 1320000 pa.

Sir, with due respect, can you suggest to me how to implement this pressure into the fluent?

• NickFL
Subscriber

Fluent, and most CFD solvers, use a floating pressure. This means that the pressure drop is calculated and not the actual pressure itself. We can do this because it is not the pressure that drives fluid flow, instead it is the gradient of the pressure. One place where the pressure will explicitly show up in your solution is when the material properties include the pressure (for example density & ideal gas). But if you are using a refrigerant with constant properties, then this is not necessary.

Quote: I am also assuming that there is no pressure loss during the study.

Are you sure? Then what is driving the flow? If you have constant properties, then simply set the velocity inlet as you have. The outlet you will set as a zero relative pressure. This is defined against the reference pressure. The solver will then back-calculate the relative pressure at the inlet. This will show us the pressure drop for the domain.

If you wanted to see the "correct" absolute pressure, then you would have to set the reference pressure to 1.32 MPa.

• pcsingh
Subscriber

Thank you for the suggestion NickFL sir, Regarding this "I am also assuming that there is no pressure loss during the study". Yes, sir, there will be a pressure loss.

@NickFL Sir, using "outflow" as an outlet boundary condition is correct or not for this problem? Please suggest.

• NickFL
Subscriber

Yes, I would avoid the outlet boundary condition. I wish they would deprecate this boundary condition or at least restrict it to the TUI.

Mathematically, for incompressible flow, one boundary condition (BC) should be a pressure and another a velocity or mass flow rate. Think back to your partial differential equations class. Remember the hyperbolic, parabolic and elliptic equations topic? This is why we had to learn that. When we move to compressible flow the momentum equations transition to hyperbolic and the characteristics of the equations let us specific two upstream BCs and that is why you see the option for supersonic pressure.

Reading back through your case, you could go with a pressure inlet and a mass flow outlet, this would be the equivalent to the velocity inlet and the pressure outlet. The key is to have a control point on both the mass and momentum equations. Depending on what is just upstream of your simulation domain, it may be valuable to have a non-uniform inlet velocity (for example: fully-developed parabolic). This would help reduce an artificial pressure drop created near the inlet.